What are Footprints and Land Patterns

Site: Teach Me Printed Circuit Board Design
Course: Learn Board Layout by Designing a Badge
Book: What are Footprints and Land Patterns
Printed by: Guest user
Date: Thursday, 9 February 2023, 12:44 AM

1. Introduction

OshPark Panel image from OshPark.com

You've no doubt seen the various metalized shapes and plated holes that are abundant on an unpopulated printed circuit board.  The size, shape, and orientation of each metalized pad on a printed circuit board is unique to the parts they are designed to hold.  Since most parts are standardized, these pad designs are standardized as well.  This book introduces the pad designs and naming scheme so you choose the right one in your next design.  And we're also going to incorporate a never-before-seen pad design for our battery selector circuit.

Hard Way Hughes"A dozen designs a day are placed on hold at Advanced Assembly due to a mismatched pattern.  DFM checks do not look for this error, but DFA checks do."

2. Plated Through Holes

Plated through-holes are little more than large-diameter vias, but they do require a small amount of design.  They have to be drilled large enough to allow the part to pass through after electroplating and have a pad large enough to allow a proper fillet to form.  You don't want to make them too large or they'll allow your part to become misaligned.

Three examples of plated through-hole parts.

The cheapest and most accurately located holes are created with drills.  So, where possible, drill rather than helically bore the holes on your PCB.  (This comment is primarily aimed at the makers.)

Just so you know -- the smallest cutters used in PCB fab shops are approximately 1 mm in diameter, so for holes smaller than 1mm, you have no choice but to drill.

Calculating Hole Size

To determine the size of the hole you need, look at the diameter of the pin you expect to insert into the board.  For rectangular parts, measure across the diagonal to determine the diameter.

For a drilled hole, IPC splits the recommended hole and pad diameters based on component density.  As density increases, so does the manufacturing difficulty.  Use the largest options wherever possible to keep your manufacturing yield as high as possible.  You should also remember that you will need an anti-pad (copper-free area) that surrounds the pad to prevent short circuits.  This number is determined by the weight of your copper.  Use your copper weight trace & space measurements to determine the anti-pad.  And if you are designing a high-voltage board, you should also look at your creepage and clearance numbers.


Hole Pad
 A - Least   Lead + 0.25 mm   Hole + 0.7 mm 
 B - Moderate   Lead + 0.20 mm   Hole + 0.6 mm 
 C - Most   Lead + 0.15 mm   Hole + 0.5 mm 

Hard Way Hughes

We haven't discussed trace & space yet.  Until we do, for this design, assume you need at least 6 mils of copper to conduct current and 6 mils of air between adjacent bits of copper to prevent short-circuits.  I'll explain the actual minimum values and how to arrive at them in a few weeks.

3. Surface Mount Basics

Understand Surface Mount Terminology

On the side/bottom of every part are a series of metalized part pins/pads that need to be connected to metalized land pads on a printed circuit board with solder.  This chapter provides a brief overview of package types and terminology.

Hard Way Hughes"In an attempt to avoid confusion in the following text, the metalized pads on a PCB will be referred to as lands or land pads while the metalized pads/pins attached to a specific component will be referred to as part pins/pads.  In real life, the distinction isn't quite as clear since both metalized parts are referred to simply as pads."

The Evolution of Parts

Integrated Circuits are available in a variety of packages.  The packages all have the same goal -- to provide an easily manufacturable way to electrically and thermally bond to a PCB.  As technology advances, the packages increase in size and pin density.

Image of Semiconductor History

A few package designs along with their timeline of introduction from anysilicon

In the early days of PCB manufacture, Dual In-Line (DIP) packaging was quite common.  Inside DIP packages, there is a silicon die that contains the integrated circuit, a metal frame, and bonding wires.  This packaging method was often standardized on 0.1" (2.54 mm) spacing.  (This is one reason why solderless breadboards evolved to have 0.1" pitch.)  As integrated circuits grew more complicated, the number of pins grew as well, which meant the packages could become quite long and wide.  Another disadvantage of DIP packages is the fact that through-hole mounting consumes a great deal of real-estate on a printed circuit board since it requires board space on every layer of a board and prevents components from being mounted on the opposite side.

One solution to the problem of limited PCB area was to use gull-wing pins on surface-mount devices.  These abandon through-hole attachments in favor of metalized lands.  Surface-mount technology allows multi-layer PCBs that don't have pesky through-holes that interfere with routing.

DIP Package

This artistic interpretation of a Small Outline Package shows the lead frame, die and bonding wires of a fictional device.

Quad Flat Packages offered a simple modification of the lead frame to add additional pins.  This technique can increase the number of pins without dramatically increasing the size of the package.

QFP28 Part

This artistic impression of a QFP28 simply demonstrates that pins extend from all sides of the package.

And as another example, Ball Grid Arrays offer even more connection points by using an XY grid of connections.  Tiny solder balls melt during reflow to connect the part to the PCB.

Ball Grid Array

This artistic impression of a Ball Grid Array offers a glimpse into the regularly spaced pattern of balls used in the device.

Our design uses a combination of package designs to allow you to learn how to work with a variety of land patterns.

4. Land Patterns

The Vocabulary of Pads, Pins, and Lands

Parts have metalized pads/pins arranged in a specific pattern called a footprint, and they connect to similarly shaped land patterns on a printed circuit board.  Land pads are always a little larger than part pads.  The slight size difference allows a fillet to form on the toe, heel, and sides of the part pins/pads that increase the mechanical strength of the connection.  It's also worth noting that many designers, including me, are guilty of using the terms footprint and land pattern interchangeably in casual conversation which undoubtedly leads to confusion.

Pad Part Pin

This image shows the terms Pin and Land that are connected by Solder

Part above Land Pattern

Land patterns generally still have the same geometric layout and centerline spacing as pads.  But individual land pads have a greater surface area than individual part pads.  The land pads are generally longer than part pads to allow for proper fillet formation

Lands come in three standard density levels that give an idea as to how much larger the lands are than the pads.

  1. Maximum Land Protrusion.  Used in low-density products where there is plenty of room between devices for large pads.  Accommodates wave or flow soldering of leadless chips, "J"-formed leads, and leaded gull-wing
  2. Nominal Land Protrusion.  Used in moderate-density products where the components are spaced close to one another, but not so close as to interfere with assembly or rework practices.  Wave or reflow soldering of leadless chip and leaded gull-wing type devices is possible.
  3. Minimum Land Protrusion.  Used in high-density products, where parts are stuffed so tightly to their neighboring parts that rework is often impossible and inspection is difficult.  These lands have the minimum possible size that still allows proper fillet formation and wetting.

These variations allow different component density, solder technologies, and rework capability by adjusting the distance the land extends around a pin/pad.

Solder Filet Formation

This animation demonstrates fillet formation on what appears to be a MLCC.  Original source unknown.

A properly designed land pattern can help to center parts that are slightly misaligned during the pick-and-place process.

resistor self centering between lands.

This animation shows a misaligned resistor self-centering during reflow.  Original Source Unknown


Printed Circuit Boards manufactured today are small, and the components often look like they are stacked immediately next to one other.  But a minimum perimeter must exist around the components that allow the part to be placed by an automatic pick-and-place machine and permit inspection and some amount of rework if necessary.  If the parts are too close to one another, it's not possible to make repairs to parts that do not bond correctly to the PCB during the reflow process.

Extending beyond the edges of a component body and its associated land pattern is an area broadly referred to as a courtyard.  IPC-7351 further subdivides the courtyard area into perimeter boundaries and perimeter areas called pattern boundarycourtyard excess, courtyard manufacturing allowance, and courtyard manufacturing zone.  These definitions can best be understood via a diagram.

Courtyard Manufacturing Zone

Image of Courtyard features from Tom Hausherr's Blog at Mentor.com

Hard Way Hughes"If all of those terms and definitions seem confusing to you, don't worry about it too much -- I work for an assembly company and the only word I ever hear is 'Courtyard' when it is used to describe the general buffer-zone around each component.  For now, leave a minimum of 1.25 mm (50 mils) of space between lands.    If you have a design that places components less than 0.5 mm (20 mils) from neighboring components, and you expect to repair/rework your product, you might have to worry about the terminology a bit more.  Otherwise, just understand you need a 'courtyard' and move on."


4.1. Land Pattern Design Shortcuts

You need an appropriate land-pattern for your part if you want the solder to properly bond your part to your printed circuit board.  That's a problem since EDA software vendors do not always maintain their parts libraries.  Before you can design a PCB, you need a library full of the parts you will use.  And your library needs land-patterns.

Find a Ready-to-Use Land Pattern

Look in your EDA Program

Database Lookup

The EDA library for your software likely has every IPC-compliant land pattern already programmed into its database.  Once you figure out where to look and how the parts are named, you should be able to find your part quickly.

Copypasta approach

Your specific part and pattern might not be present, but there's a good bet that the land-pattern for it is.  You might be able to find a similar part and copy the land pattern into your library where you can edit the pins and link it with your new schematic component.

Pattern Wizard Approach

Many EDA programs now offer "pattern-wizards" that generate IPC-7351 compliant land patterns.  If your EDA software offers a wizard, it might be worth spending a few minutes learning how to use it.

Look at your Manufacturer/Distributor Website


Manufacturers will occasionally offer a land-pattern as part of the digital downloads for the part on their website.  It's not too common, but it does occasionally happen.

Distributors & 3rd Part Vendors

Manufacturers should absolutely release a land pattern and a 3D model with every part they produce, but they don't.  So services such as Octopart, SnapEDA, PCBLayout, etc... pick up where they left off.  The 3rd party vendors make the patterns available either as a service or at a fee.  Distributors such as Digi-Key then link to the pattern on their product page.

4.2. Provided Land Pattern Accuracy

Land-Pattern Double-Check

Creating land-patterns is one of the more tedious aspects of electrical engineering.  But sometimes you just have to sit down and do it.  It's also worth noting that you will often find mistakes in the land patterns you find in online-libraries, which should further motivate you to create your own libraries of custom parts.  As an example, the land-pattern for the BNO055 we sourced for this design was originally identical in size and shape to the footprint of the BNO055.  

Page 102 of Bosch-Sensortec's BNO055 datasheet (bst-bno055-ds000.pdf) provides a somewhat intimidating amount of information about the footprint dimensions.  But there is absolutely no information about a suggested land pattern name, no information on how to go about creating a land pattern, or where on the Bosch website an appropriate land-pattern might be found.

Footprint dimensions for BNO055

The engineers at Bosch apparently expect PCB designers to take the information from this diagram and use the equations from IPC-7351 to design or create an appropriate pattern.  

I imagine whoever made the land pattern that Bob and I initially found was so focused on deciphering the information from the datasheet that they missed the fact the land pattern wasn't present at all, so they created a 1:1 copy.

While the centerline spacing for the rows and columns of pads will be a 1:1 copy, land pads are always bigger than part pads.

5. 2-Lead Discrete Components

In Chapter 5 of What is Circuit Design, I introduced E-Series and component value standardization.  What wasn't explored at the time is that those components are also standardized around common sizes.  

Hard Way Hughes

"Diodes, chip capacitors, resistors, and inductors all come in common sizes.  In the United States, it is common to hear engineers mention "0603, 0402, 0201, 01005" sizes, referring to the imperial component dimensions."

Imperial and Metric Component Sizes

A collection of common part sizes as measured in imperial and metric measurements

Unfortunately, in North America, the parts are often listed in catalogs and online part libraries based on their size in imperial measurement (measured in tens of mils) while their footprints and associated land patterns are defined in metric measurements (measured in tenths of a millimeter.)  And to make matters worse, many of the metric values are rounded to make them identical to imperial values for different size parts.  Currently, in America, engineers describe parts based on their imperial sizes, but you must use their metric footprint to make the land patterns.  


A select number of parts that have similar or identical values across the different measurement systems.

You might remember that earlier in the course, we selected a 0.1 uF 0603 ceramic capacitor.  The 0603 referenced its length and width in imperial measurements - 60 mils long by 30 mils wide.  However, the footprint we need to use for this part is 1.6 mm x 0.8 mm -- we'd choose a CAPC1608x90

Hard Way Hughes"We put jobs on hold every day because engineers pick parts that don't fit into a particular footprint size."

6. Package Name Resources

Images from SparkFun

Images of various packages and their names from Sparkfun.com

Hard Way HughesThe names of various packages can be found all over the web, but I was unable to find a single comprehensive source (not covered by copyright) in two hours of searching -- let me know if you find one that we can share in the course.  You do not need to sit down and study these patterns and names -- you will pick them up naturally over time as you gain familiarity with the assembly space.

Here are a few additional resources to get you started.  The list is far from comprehensive.


Texas Instruments

Their page http://www.ti.com/support-packaging/packaging-tools/find-packages.html sorts their parts based on the package type.


And their document http://www.ti.com/lit/sl/sszb138a/sszb138a.pdf lets you find the relationship between a package name you are familiar with (e.g. BGA, QFN, SOP) and their proprietary part naming / numbering scheme.  


https://www.nxp.com/packages provides a search page that will locate a datasheet specifically for each package they manufacture.

Analog / Linear

Provides engineering drawings for each package at https://www.analog.com/en/design-center/packaging-quality-symbols-footprints/package-index.html.

3rd Party

  • Ultralibrarian.com provides excellent 2D images along with downloads for the three density levels.


6.1. Land Pattern Determination

The Old Way

The size and shape of discrete components, including chip resistors and their associated land patterns, have been standardized for a number of years.

Component and Land Pattern

These values are copied from IPC-SM-782A rev 2 from 1999.  This data precedes the subdivision into maximum, nominal, and minimum density classifications.  Measures C and Y are redundant.

You'll notice that IPC dictates both the size of the part to the manufacturer and the recommended land pattern to the PCB designer.  Take package 3216 (1206), for example.  The length is 3.2 mm ± 0.15 mm and the width is 1.6 mm ± 0.15 mm.  The nominal length and width of the footprint, measured in tenths of millimeters, are used to generate the metric package number 3216.

The New Way

Things have become more complicated though, since the introduction of the maximum, nominal, and least density specifications.  Now each part has three land patterns associated with it. Each pattern describes the board density, land pad size, and courtyard.  The maximum variant offers the greatest capability for cleaning, rework, and inspection.  Components that use the minimum variant are packed so tightly next to one another that there is often no opportunity for repair or rework.  Many discrete components (inductors, capacitors, resistors, diodes, etc...) have similar land pattern dimensions and similar naming schemes.

Maximum Nominal and Least density patterns.

Land-patterns (including courtyard) for a molded 3216 polarized capacitor are CAPPM320X150X180L80X120M, CAPPM320X150X180L80X120N, and CAPPM320X150X180L80X120L

You should be able to find land patterns for your discrete parts without too much trouble.  Remember, you can use your footprint wizards, or copy the pattern from another part if you have to add parts to your library.

7. Land Pattern Naming Scheme

If you can find the package name of your part, either in a datasheet or at a distributor website, you can start to generate and organize your own footprint library.  

This document (from PCB Matrix Corp, now Mentor) provides the IPC-7351 naming scheme for each package type.  I'd recommend looking it over to get an idea of how the land pattern names are produced.